Introduction to the Haas CNC Control

Sun, Jun 6, 2010

Control Tips, Expert Tips

Haas owners and operators have known for years how easy the Haas CNC is, but now the word is out. An independently published market survey showed industry professionals rating the Haas control as the most user-friendly control they’ve worked with. We’ll show you some highlights throughout this post.Introduction to the Haas CNC Control

Introduction to the Haas CNC ControlThe cursor arrows and the PAGE UP and PAGE DOWN keys get a lot of use when you’re navigating the various Displays on a Haas control. To find a particular machine setting in the Settings display, for example, you just type the setting number in the input buffer and hit the down arrow. The PAGE UP / DOWN keys, obviously, take you to either the previous or the following page in the display.Introduction to the Haas CNC Control

  • The PRGM display shows the current (active) program.
  • POSIT shows you 4 different position displays to show true and reference positioning.
  • Manage tool, work and wear OFFSETSs easily.
  • Paging Up and Down in the CURNT COMDS displays a complete list of info about the machine, as well as the active program.
  • The machine sends messages to the operator using the ALARM display
  • You can post your own messages on the MESGS display.
  • Haas Service Techs use the Parameters & Diagnostics displays.
  • SETNG lists machine Settings (change them as needed), and the GRAPHICS display lets you avoid crashes.
  • HELP/CALC is where you get answers.

Program Review

In the PRGRM display, Program Review allows you to cursorIntroduction to the Haas CNC Control through and review the active program on the right side of the display screen, while also viewing the same program, as it’s running, on the left side of the screen. To bring up Program Review, press F4 (you must be in MEM mode).

Background Edit

This feature allows you to edit a program (in MEM mode) from the PRGRM display while a program is running. Type in the program number you want to edit (Onnnnn) and press F4. You can then do simple edits (INSERT, ALTER, DELETE and UNDO) either to an existing program, a new program or even the program that is presently running. However, edits to the program that is running will not take effect until that program cycle ends with an M30 or RESET.

Position Display
Quick Zero on DIST-TO-GO Display

You can use the Distance To Go screen to quickly zero out the Position displayIntroduction to the Haas CNC Control for a reference move. When in HAND JOG mode and in the Position display, press any other operation mode key (EDIT, MEM, etc.) and then go back to Handle Jog. This will zero out all axes on the DIST-TO-GO display, and begin showing the distance moved.

To Zero the POS-OPER Display

This display is used for reference only. Each axis can be zeroed out independently, to then show its position relative to where you selected to zero that axis. To zero out a specific axis, PAGE UP or PAGE DOWN in the POSIT display to the POS-OPER large-digit display page. When you Handle Jog the X, Y or Z axis and then press ORIGIN, the axis that is selected will be zeroed. Or, you can press an X, Y or Z letter key and then ORIGIN to zero that axis display. You can also press the X, Y or Z key and enter a number (X2.125), then press ORIGIN to enter the number in that axis display.

OFFSET Display

Pressing the OFFSET key repeatedly will toggle back and forth between the Introduction to the Haas CNC ControlTool Length Offsets and Work Zero Offsets pages.

Entering Offsets

Pressing WRITE/ENTER will add the number in the input buffer to the cursor-selected offset value. Pressing F1 will replace the selected offset with the number in the input buffer.

While F1 will set the entered value into the offsets, F2 will set the negative of the entered value into the offsets.

Coolant Spigot Position – The coolant spigot can be programmed to move to the location entered in the Offset display (Tool Offset page, Coolant Position column). The coolant nozzle can be adjusted to one of 10 positions for each tool – position 1 is the highest, 10 is the lowest. The nozzle will shift to that position whenever an M08 or Hnn code is encountered in the program.

Clearing All Offsets and Macro Variables – In the Tool Length Offset display, you can clear all the offsets at once by pressing the ORIGIN key. The control will prompt: “ZERO ALL (Y/N)?” to make sure this is what you really want to do. If Y is entered, all the offsets in the area being displayed will be zeroed. The Work Zero Offset page (and the Macro Variables page in the CURNT COMDS display) will do the same thing. (Any Mill Control ver. 10.02 and above; any Lathe Control ver. 3.00 and above)

Up to 200 Tool Offsets

Haas mills now offer up to 200 tool offsets, double the number in previous versions. (Any Mill Control ver. 10.22 and above)


The first page of the Current Commands display shows 15 lines of the active pIntroduction to the Haas CNC Controlrogram, as well as feedrate and spindle speed. The column on the far right shows programmed feed and speed (PGM Fnnnn, PGM Snnnn), actual feedrate (ACT Fnnnn), commanded spindle speed (CMD Snnnn) and actual speed (ACT Snnnn).

Actual speed and feed values are just that – what the spindle and feedrate are really operating at with any adjustments using the Override keys. In addition, this page shows spindle load, axis loads, surface speed, chip load, and spindle CW, CCW or STOP commands. Current axis positions are shown in the upper right corner. Change the coordinates displayed (Operator, Work, Machine, or Distance to Go) by using the cursor up and down keys.

Tool Life Management

In the CURNT COMDS display, you can PAGE DOWN to the Tool Life management page. On this page, the Usage register increases by 1 every time that tool is called up in the spindle. Enter the number of times you want that tool to be used in the Alarm column, and when the Usage number for that tool reaches the number of uses in the Alarm column, it will stop the machine with an alarm. This helps you monitor tools to prevent them from breaking and parts being scrapped.

Tool Load Management

The next PAGE DOWN in Current Commands will bring you to the Tool Load page. Spindle load condition can be defined for a particular tool, and the machine will stop if it reaches the spindle load limit defined for that tool. A tool overload condition will result in one of four actions by the control; the action is determined by Setting 84. ALARM will generate an alarm when overload occurs; FEED HOLD will do just that; BEEP will sound an audible alarm; or AUTOFEED will automatically decrease the feedrate. This also helps you monitor tools.

Clearing CURNT COMDS Values

The values in the Current Commands display pages for Tool Life, Tool Load and Time registers can be cleared by cursor-selecting the one you wish to clear and pressing ORIGIN. To clear everything in a column, cursor to the top of that column (onto the title) and press ORIGIN.

ALARM / MESGS Displays
Alarm History

Pressing the right or left cursor arrow while in the Alarm display will list the last 100Introduction to the Haas CNC Control alarms, with date and time. Use the cursor up arrow to see the earlier alarms. Pressing either the left or right arrow again will bring you back to the normal Alarm display.

Alarm History saved to RS-232 and Disk – This is a new feature. From the Alarm History screen, the alarm history (the last 100) can be saved to a floppy disk by entering a file name and pressing F2. Alternately, the alarm history can be sent to a PC by pressing SEND RS232. The output from either method will contain a percent sign (%) on the first and last lines. (Any Mill control ver. 10.22 and above; any Lathe control ver. 4.02 and above)

Leaving Messages

You can enter a message in the Messages display for the next person, or for yourself. It will be the first display shown when you power up the machine, IF there are no alarms other than the usual 102 SERVOS OFF alarm. If the machine was powered down using EMERGENCY STOP, the Messages display will not show up when you turn the machine on again. Instead, the control will display the active alarm generated by the emergency stop. In this case, you would have to press the ALARM/MESGS key to view a message.


Changing Parameters – Parameters are seldom-modified values that change tIntroduction to the Haas CNC Controlhe operation of the machine. These include servo motor types, gear ratios, speeds, stored stroke limits, lead screw compensations, motor control delays and macro call selections.

Modifying some of these functions will void the warranty on the machine. If you need to change parameters, contact Haas Automation or your dealer. Parameters are protected from being changed by Setting 7. Be sure to download and save a copy of your machine parameters so you’ll have a backup if needed (refer to the LIST PROG section to see how to save your offsets, settings and parameters to a floppy disk).

The Diagnostics display is used by Haas Service technicians to check the status of the machine for diagnostics and servicing.

Graphics Display
Zooming in

In the Graphics display, use F2 to zoom in on the graphic. After pressing F2, press PAGE DOWN to zoom in further and PAGE UP to expand the view. Use the cursor arrows to position the zoom window over the section of the part that you wish to view in close-up.

Press WRITE/ENTER to save the new zoom window, and Cycle Start to see the close-up graphic run. Press F2 and then HOME to get back to the original full table view.

Settings Display

Because the settings give users a great deal of powerful and helpful command over the control, we recommend reading the entire Settings section of the operator’s manual. Go here for some examples of how useful they are.

HELP / CALC Displays
To see a list of all the G and M codes available for the machine, press HELIntroduction to the Haas CNC ControlP and then the letter C. Press the letter D for a list of all the subject areas available in the Help directory; then select the subject you want by pressing the indicated letter. Press HELP/CALC again to access the calculator.

Transferring Simple Calculations

In the Trigonometry, Circular or Milling and Tapping calculator, the number in the simple calculator box (in the upper left corner) can be transferred down to any cursor-selected data line. Cursor to the register you wish to transfer the calculator number to and press F3.

Transferring Calculated Values

You can transfer the highlighted value in a Trig, Circular, or Milling data register into the calculator box by pressing F4. Use the up and down arrow keys to select the data registers, including the calculator box, and the left and right arrows to select LOAD + – * /. To enter a highlighted data value into the calculator box, LOAD must be selected when you press F4. If one of the operations is selected, pressing F4 will perform that operation, using the number in the highlighted data register and the number in the calculator box.

Transferring to EDIT or MDI

In either EDIT or MDI mode, pressing F3 will transfer the number in the calculator box (when the cursor is on the number in the box) to either the EDIT or MDI input buffer. You will need to enter the letter (X, Y or Z) you wish to use with the number from the calculator.

Circular Calculator

The Circular calculator will list four different ways that a circular move can be programmed using the values entered for a calculated solution. Four different program lines for executing the circular move will be listed at the bottom of the display. One of the four program lines can be transferred to either EDIT or MDI.

1. In the circular calculator, cursor onto the program line you wish to use.
2. Press either EDIT or MDI, where you wish to insert the circular move.
3. Press the F3 key, which will transfer the circular move that you highlighted into the input buffer line at the bottom of the EDIT or MDI display.
4. Press INSERT to add that circular command line into your program.

One-Line Expressions

A new feature of the Calculator display is that it will now evaluate a simple math function (previously, it was only possible to enter a number into the input line). Enter a simple, one-line expression without parentheses, such as 23*4–5.2+6/2. It will be evaluated when the WRITE/ENTER key is pressed, and the result (89.8 in this case) displayed in the calculator box. Multiplication and division are performed before addition and subtraction. (Any Mill Control ver. 9.49 and above; any Lathe Control ver. 2.24 and above)

|| More